How to set parts AREA iProperty to display in Title Block in square meters?

[MagnusD]

Hello, recently i posted this on official autodesk discussion, but without any answer, so I'm trying here

 

 

For product cost calculation process I'm trying to help my collegues by placing area value of a part/element/product into documentations TitleBox, it's for determining how much paint is necessary for the particular product.

 

 

Inventor 2011 enables to insert parts iProperties Area value into the title box but the default units of AREA iProperty in inventor 2011 is square milimiters, when You get it to show in Title Block it looks like this 123123,0000 mm^2 (the values are for reference only)

 

I'd like it to look like this 0,1231 m^2 (at least)

 

Through iLogic I managed to get the area value to be inserted into a custom iProperty (in the parameter list (fx)), there I changed the units into meters, but I don't know how to configure my Documentation Template, to put that value into the title block.

I'm new to iLogic, and I'm not familiar with VisualBasic, so I use iLogic only with "web search engines" , when I can't find what i'd like iLogic to do i ask for help.

 

 

I searched the community for some resources how to put a custom part parameter into Title block, but I couldn't find anything.

 

Regards.

 

 

[Tony2178]

Hello,

 

We are attempting to create a similar scenario, only with sq inches to sq Feet. Would it be possible to see your iLogic code, as we may be able to help you accomplish getting the info into your Title Block.

 

Thanks

 

Anthony

[MagnusD]

Hi, first of all sorry for the delay, my posted reply had links to imageshack, and propably was waiting (or still is) to be moderated, so I posted again, and pasted the pics manually.

 

I already managed to do what I wanted, but havent updated the thred about it, sorry for that.

(forgive me my rough english It's not my native)

 

Here Are some screens

 

1. In the parts/assembly file (template file) I created a custom parameter of desired name, in my case "p_area" and I defined it's units to what I needed, that is square meters, then I checked the Export box and defined more options from the right click custom properities of that parameter.

 

2. then I created a simple iLogic rule named "iProps" You ofcourse can make it an external rule ofc.

p_area = iProperities.Area

 

 

 

basically it transfers the area value from parts iProperities into my custom parametr in (fx) parts parametes list

 

3. then I defined the rule execution triggers, whenever the geometry changed the rule would recalculate the area value, so it would be always accurate, its in Management tab (at least that's the direct translation of the tab from Polish) iLogic section. I checked the before save trigger too, just to be sure.

 

 

4. I opend the IDW template and inserted a base View of the part with the iLogic rule into the drawing

 

 

5. I opened the table box Definitions (sketch) and added a text field, then I chose in the TYPE dropdown menu list the "Custom properities - Model" (at least thats the direct translation) and in the nest dropdown menu i chose my custom parameter

 

 

 

6. Closed the Table Box Editor, remooved the Base View and saved the IDW as a template.

 

This method gives You control of units display of the particular parameter in model/assenbly file, I turned it off becouse I dont like the "^" mark so I manually added m2 (the 2 as a uppercase),

 

 

Unfortunately You have to manually add the properity "p_area" to custom properity list(fx) and set the "want to be" units, ofcourse if You can code that in iLogic, You can make it by iLogic, I can't

the rule could be set as an external rule if it could do all of the things, without manually adding the parameters to custom parameters list in inventor and the iLogic triggers Anyway I'm content.

 

I hope it helps You.

 

If anything is not clear due to my lack of skill in grammar or generally english dictionary feel free to ask.

Regards

MS